Axisymmetric model with elastic foundation

[kichwa]

Hi

I’m new to ANSYS and have previously written my own FE code in Fortran. Now I’d like to use ANSYS to verify an FE model in Fortran but am not sure how to go about it.

The model is as follows: An axi-symmetric model of an elastic circular slab on an elastic foundation. I have used triangular, three noded plane-stress elements (2 dof per node) which are being rotated around the central axis. The slab is restrained horizontally on its circular boundary (for the development of membrane action) and is subject to a small distributed, circular load in its centre. The stresses recovered are as follows:

Sigma_r
Sigma_z
Tau_rz
Sigma_t

Where: r denotes radial direction, z is vertical and t is tangential.

I would like to model it in the same fashion using ANSYS with the same triangular elements (Complete with Winkler Spring foundation whereby I can specify a foundation stiffness in N/m^2/m).

Once I have set this up, I’d like to compare the results with those of my Fortran program to see if it’s accurate.

Any advice on this would be greatly appreciated!

Thank you in advance.

 

[kichwa]

Once I've defined the area, the elements, material properties etc and meshed it, how do I add an elastic foundation? Would this foundation be modelled adequately by link elements attached vertically to the foundation nodes?

 

[cbrn]

Hi,
there are some element types which incorporate Elastic Foundation as a keyoption / real constant.
I don't remember which ones, however.

Alternatively, you can set up spring elements COMBIN14. Links could also possibly be used, but they would be much more difficult to set up. The right combination of keyoptions and real constants are all you need with COMBIN14, so I'd go with them.

Regards

 

[kichwa]

Thanks cbrn. I'll use COMBIN14. However the problem now is that I'm not finding the help files useful for setting up the problem.

Could someone PLEASE outline the steps for me. Here's what I have so far:

I've created an area as follows: Preprocessor - modeling - create - areas - rectangle - by dimensions

Then I chose my elements as follows: Preprocessor - element type - add/edit/delete - add - {then I chose PLANE2} - options - {i chose the axisymmetric option}

Then I chose COMBIN14 as well and in options, selected longitudinal y dof

Then I meshed it as follows: Preprocessor - Meshing - Size Cntrls - Manual Size - areas - all areas - {then I entered my element edge length. Then Mesh Tool - mapped - mesh - {then I clicked the area and hit ok}

Preprocessor - Material props - material models - structural - linear - elastic - isotropic - {Then I filled in young's modulus and poisson's ratio}

I have no idea what to do now. How do I assign those material properties I chose to the triangular elements? How do I add the springs? How do I give them a k value? How do I restrain the bottom of the springs while having the tops attached to the underside of the solid?

I don't know anyone who used ANSYS so have nobody to ask. While my queries may seem elementary, any help would be greatly appreciated.

Thanks.

 

[dannyj]

Hi. If it's a 3D problem you have to switch from plane 2 element type to a more appropriate element type, like shell 43, shell63, shell 181 etc. After that you have to create a real constant which is basically the thickness of the plate.
After creating the material you to assign these properties to the surfaces. To assign these properties to a surface you have to go to /preprocesor/meshing/attributes/picked area or all area (depends on the areas you want to a assign a specified property). All elements created on that surface will have the properties given by you. To create a combin14 element, you have to define two nodes. For your problem, after you create the fe model for the surface, just copy the nodes from the surface to a location bellow, in this way every node on the surface will have a corespondent node. Then you create the combin 14 element type. After that go at real constant and create a real constant for combin14. Here you can enter the k coefficient. In order to create the elements, first you have to switch from the implicit values assigned by ansys for creating a element to the one that you desire. Go under meshing/mesh attributes an change the global for element types and real constant(combin 14 and real constant set 2, lets say). Then you have to create the elements by picking. You can do this in to ways:
1. issue the e,p command
2. preprocesor/create/elements/autonumbered/thru nodes (does the same think as e,p)
To restrain the nodes, go under solution/loads/apply/displacements, select the nodes, choose the degrees of freedom you want to restrain and put 0 at the value.
Hope this will help you.

Regards